SMD Mouting hole using a captive Screw - past mask file
For one of our design and to fix my PCB I'm using a captive screw from We elektronik Ref 746 600 330R. When I generate a plot file, I discover that in the past mask file I find a hole for the SMD captive screw and not just the solder pad.
Is there any solution ?
Thanks for your help.
CommentsAdd a comment
UPDATE: After investigating further, I managed to create a component in the library which provides the correct paste mask, solder mask and none plated hole as confirmed by the Gerbers in ViewMate. It was an iterative process working with the original component download from SamacSys and I will try to reproduce my steps and produce a technical note on the process.
Attached is my PCB file from which you should be able to extract the footprint and update the component from SamacSys.
The basic steps were to create the required paste mask openings on the documentation layer by copying and pasting from the PCB editor. Then in the component footprint editor change the layer from documentation to paste mask.
The following is my solution for this, but there will be alternatives.
For this type of footprint requiring openings around the hole for paste but to block the hole, I tend to work at the PCB level rather than in the library. I learnt this from the Fiducial FAQ where I found it quick and easy to copy from a set of reference symbols and paste to the working PCB rather than attempting to get around the library component restrictions.
Using a PCB with solder and paste mask layers, I added a pad of the required size and using the pad properties set it for Top Copper, I also set it for not plated, but it always seemed to default back to plated later!
Next I created the paste cutouts using the closed shape for one quadrant and setting the sides to arcs (it was done by eye just to illustrate). The filled shape was copied and pasted 3 further times to the required orientation.
The solder mask cut out was just a filled circle.
Attached is my demo PCB file just to illustrate my method. Brad may show how to do this as a component which could be more convenient.
The image is the solder mask and holes in a Gerber viewer.
I don't know whether you created a DS PCB component/footprint for the captive screw, or just added a pad to the board. I did a search using the library loader to see if a component for this Wurth part was already available for DS PCB. There wasn't, so I went ahead and requested one be created. (This is something any user can request.)
The data sheet for the part calls for less than full paste coverage, as well.
There are ways to achieve that in DS PCB, but it is an issue best discussed in the support forum for DS PCB. Here is one previous thread there that touches on the topic: https://designspark.zendesk.com/hc/en-us/community/posts/360005820494-Solder-paste-override
@BradLevy you must have just missed it. From my request I was notified it was available at Wed 03/04/2019 16:40. I have not investigated yet, but PCB Part Library components are restricted to what can be directly created within DesignSpark PCB, so the part may require modifying to create the required paste mask.
Having checked the Samacsys part it also has paste covering the hole. I have asked if this can be updated to the required paste openings but this may be a DesignSpark PCB limitation and require manual editing of the mask.
@RS Components Support Yes, it was just under an hour from the time I requested the part creation to the email notifying me the part was ready. I check out the Samacsys part yesterday after the notification and saw that it had paste covering the hole, which I reported to them. I also noticed and reported to Samacsys it looks like they used a plated hole, while the Würth Elektronik data sheet calls for an unplated hole. It will be interesting to see any followup by Samacsys. I know paste mask refinement is one of the more limited areas of DS PCB. I'm often able to find a way to accomplish the intended coverage, but sometimes the techniques (copper shapes overlapping smaller pads) generate DRC errors in situations which are actually safe but for which there is not a way to communicate sufficient info to the design rule checking for it to realize it is safe and shouldn't be flagged. If I get a chance later, I might try creating one that way for this part. I realized yesterday that the four non-paste spokes on the Würth datasheet's footprint were probably not there for paste reduction, but to provide physical support/connection to the masking over the hole, a limitation that photo-imaged silk screen text or solder mask layers don't have.
@BradLevy SamacSys have confirmed that the custom paste openings cannot be supported within a DesignSpark PCB component. If you create a library component it would be helpful if you would publish this as an article.